| T O P I C R E V I E W |
| smholley |
Posted - 11 Mar 2014 : 20:39:05
I have a schematic which uses net reference symbols for 0v and 3.3v. All was well until towards the end of laying out the PCB the two nets seem to have merged and I can find no way of de-merging them. If I rename a section with a new net name it renames all the 0v and 3v3 points with the same name.
Any suggestion how they became merged to start with and how I can recover the situation without starting from scratch .
|
| 7 L A T E S T R E P L I E S (Newest First) |
| edrees |
Posted - 18 Mar 2014 : 17:48:02
Not when they are (unintentionally) different nets on the schematics, hence the suggested use of net colours, so they are instantly recognisable, i.e. Green for 0V, Red for 5V, Blue for Raw_DC etc. without the need to find the Net name (which can be moved "accidentally" without ones knowledge).
|
| Iain Wilkie |
Posted - 18 Mar 2014 : 13:58:52
Connectivity check will show any split or unconnected nets.
Iain |
| rvpilot |
Posted - 18 Mar 2014 : 12:15:21
Just another handy tip ...
On my schematics I always go to Display settings and allocate unique colours to the common nets, i.e. GND, VCC, 3V3, etc. You can then see at a glance that the sub-net is connected to the right net and I also show the net name as a backup.
It's also a very useful validation when the net spans multiple schematic sheets.
I've been caught out a few times when I've got a board back from the PCB manufacturers to find a split ground or power net !! ... Never again :-) |
| jlawton |
Posted - 15 Mar 2014 : 21:27:47
It's ok if you use blank voltage references (create your own) and then change the net to the one you want. Always display the Net Name to prevent errors.
The golden rule is to never copy and paste a reference unless you are absolutely clear it is on the net you want.
John Lawton Electronics |
| smholley |
Posted - 12 Mar 2014 : 11:05:10
Useful replies both.
Thank you for your help |
| Iain Wilkie |
Posted - 12 Mar 2014 : 10:10:51
I NEVER use these things ..... you can make mistakes that are not obvious. I simply create a little T junction at the end of any power net and then display the net name and place it on top ... that way you cannot go wrong.
Iain
|
| edrees |
Posted - 12 Mar 2014 : 09:28:17
You may have copied a ref symbol which has become detached from its net name, and when you copied it to another part of the circuit, EPC allocated a new name for that net (it may have asked you to confirm the two nets will be joined). A 0V schematic symbol can for example be connected to +5V net. Or you have possibly inadvertently shorted the two tracks together on the pcb editor (again it should have warned you).
If the schematic is correct then just perform an Integrity check on the pcb and follow the corrections offered. Otherwise,-
Go back to your schematic and highlight each 0V net, and then rename net to appropriate name, (Change Name Of Subnet Only, -NOT globally). The schematic is the "Master" here. I find changing the net colour helpful here. Allocate two different colours for 3V3 and 0V to confirm all nets have been changed correctly.Then perform a forward design change, and the pcb will loose all the incorrectly linked nets. |
